Learning Forum

[shamik062]

Hello Everyone,

I am doing a prestressed Explicit Dynamic Analysis Where the results of bolt prestress in Non-Linear Static Structural is used as setup of Explicit Dynamics (Workbench Autodyne). When I am Trying to Solve the Static Structural simulation I am getting the following error.

[peteroznewman]

You have a Near Open contact. That causes the Static Structural model to fail to solve.
Go to that contact and set the Interface Treatment to Adjust to Touch
Under Analysis Settings, use 100 Initial Substeps.
That will allow Step 1 to converge.

[shamik062]

Thank you so much for your help. I incorporated the changes that you mentioned and now the Static Structural Simulation is solved. But now there is a new problem regarding the Explicit Dynamics Analysis which is using the result of this Static Structural as the prestressed condition. Please note that for Explicit Analysis, only Workbench Autodyn is available to me.
First of all I am getting the Warning related to several Bonded Contacts that I have used in Static Structural Analysis. The images of the warning is attached below.
From the deformation plot of Static Structural Analysis it can be seen that there is 0.8 mm of maximum penetration between the rubber. Is that causing these warning message? I have attached the image of the penetration plot below.
To eliminate the penetration, I have tried to change the formulation of the bonded contact to Normal Lagrange. But in that case Static Structural Simulation is not converging.
Secondly the stress in the bolt should increase from Static Structural result when the impact occurs. But the stress result I am getting is unrealistic. The max stress is at the start of the explicit simulation and then it just fluctuates. The images is attached below.
Also the Kinetic Energy of the System should be constant before the impact since only the ball is moving with a constant velocity. But that is also fluctuating as shown the below image
I am actually new to explicit dynamic simulation. So I can not figure out what I am doing wrong.
If you can kindly look into this problem that will highly helpful.
Thanks in advance.
I have attached the updated achieve file (Static Structural Solved) below.

[peteroznewman]

Step 1. Replace all Bonded Contact with Shared Topology. In Mechanical, delete all Bonded Contact. Open the geometry in SpaceClaim. Put all the parts that are to be bonded together into one Component. Open that Component, go to the Workbench tab and click the Share button. Now in Mechanical, meshing will connect parts using shared nodes at the interface. The only contacts are Frictional.
Step 2. Understand Static Structural Pre-stress behavior in Explicit Dynamics. Suppress the two balls. Observe the behavior of the system in the Explicit Dynamics solution. Is it behaving well?
Step 3. Unsuppress the two balls and run the Explicit Dynamics solution.

[shamik062]

Thank you for your reply. I did what you advised. I replaced all the bonded contact with Shared topology and solved the Static Structural Simulation without any issue.
Next I have dragged and dropped all the boundary condition (Including the fixed support on ball) from static structural to Explicit Environment. I think that is equivalent to suppressing the two balls since its basically fixed. Then I ran the Explicit Analysis.
The analysis terminated very quickly after a couple of cycles with message " Energy error is too large".
I changed the maximum energy error to 10 and reference energy cycle to 1e+07, just to run the analysis till end. The analysis did come to the end time that I have specified (0.001 sec)
Now the displacement as well as the stress plot is that I am getting is very strange. The Bolt is splitting into two and going upward from the plane which I had specified during the Static Analysis to apply the bolt pretension. I know that the bolt pretension object splits the bolt shank into two and pulls them towards each other in order to apply the pretension load. But I have no clue why this strange phenomenon is occurring in explicit dynamics. I have attached below the images of the displacement and stress result of explicit analysis at the end time. I cant paste the images in the comment box for some reason. So I am adding them as attachment.
I did not ran the analysis with balls unsuppressed . I have attached the updated archive. In project schematic page, block D,E,F contains the latest analysis with shared topology
Can you please take a look into the analysis and help me solve the problem?
Many thanks for your help.

[peteroznewman]

What initial velocity will you apply to the balls?
Why did you choose Explicit Dynamics over Transient Structural?
I recommend you first try Transient Structural. In the example below, I have created a 1 m/s downward velocity.
To simplify this model, I suppressed Bolt Pretension. That can be unsuppressed. The Analysis Setting needs to have a first step to load the pretension and a second step where it is locked, both of which have Time Integration turned off.

[shamik062]

Sorry for my late reply as I got occupied with other job.
The initial Velocity of the ball ranges from 10m/s to 15m/s depending on the various design parameters. Actually I do not know how to run static simulation in transient dynamics environment and that is the issue I am facing with model you have provided. The same model that converged in static structural analysis now is not converging in transient dynamics system.
I have unsuppressed the bolt pretension and turned off time integration from Load Step 1 and 2
. I have the following settings for the first two load step (i.e. Bolt Pretension and Lock):
Load Step -1

Load Step-2
Load Step -3 I did not change the Time Step that you originally provided. I just changed the end time.
But the load step 1 and 2 are not converging and giving me element distortion error.
I also have another query regarding the model that you have provided.
Why it is necessary to apply initial velocity to nodes. Can't I apply the velocity to the surface?
If I want to apply the velocity according to some user user defined co-ordinate system, can that be done?
Kindly take a look at the attached achieve and help me solve the problem?

[peteroznewman]

Once you turn off Time Integration, the model is like a Static Structural solution. I don't have time to look at your model now, maybe later. Anyone else is welcome to help out here.
If you apply the velocity to the surface only, the nodes and elements on the interior of the balls have zero velocity. This will cause stress to develop in the ball in the first time increment. If you apply the velocity to all the nodes in the ball, then the entire ball will move uniformly in the first time increment.
I expect if you create a coordinate system, that you can use that to define an initial velocity.
Pay attention to the way in which initial velocity is defined in Transient Structural because it is not obvious. You apply a Displacement d in a step that has a time increase of dt from the previous step end time. Therefore v = d/dt is the initial condition for the next time step.

[shamik062]

Thank you for your tremendous help in this topic. I will try to solve the convergence issue and let you know about the progress. Yes the method of defining the initial velocity is different here and thanks again for providing clarity on that.

[shamik062]

Hi Peter. I actually managed to solve the problem. The issue of Non Convergence in the implicit part was due to the fact that the bolt prestress load was being applied in stepped configuration. That was needed to change into ramped configuration. To do that I inserted a command object with kbc,0. This set the load application into ramped configuration and the implicit part converged without any issue.
Regarding the application of velocity I looked into the Mechanical User Guide. For my case I inserted two additional step (After the Bolt Pretension Step and Lock Step). My complete load step looked like following image :
But the trick is I need to deactivate the last load step so that the ball moves freely in Y direction with the velocity defined in "Velocity Initiation" step, which in my case is 12 m/s. With this method the analysis completed without any issue.
Thanks peter for your help in this project. I am marking this discussion as solved and closed.